CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)

 muralikiran85 October 29, 2013 12:00

Hi all,
I am a master student doing my thesis in icem cfd. I need to do hybrid meshing(structured and unstructured). I got a link (http://alexanderblack.co.uk/cfd/hybrid-mesh-in-icem/) regarding it. while doing it accordingly i got problem in merging nodes. can anyone help me in hybrid meshing. if possible can anyone explain me the procedure in detail, about how to do hybrid meshing.

Warm Regards
Muralikiran Krishnakumar
muralikiran85@hotmail.com

The process of hybrid meshing is described pretty accurate in your link. The most important points of hybrid meshing are equal mesh sizes and quad aspect ratio near 1 on the interface. Heres how I do it:

1) Create two separate geometries from the original geometry. one for hexa one for unstructured. I usually choose the interface to be plain. Further there are no prisms allowed on the interface. So I put it in location that allows to use prism for most of the unstructured part. The most obvious spot for the interface is not always the best. There can also be other restriction like wall distance. For geometry preparation Design modeler is very useful.

2) Create hexa mesh for hexa part with respect to restrictions above and save it as xxx.uns.

3) Create unstructured mesh via Octree -> delete volume ->smooth surface -> Delaunay -> smooth volume -> prism. Smoothing has a huge effect on prism generation. Laplace smoothing gives you a very uniform distribution. So it might also have a positiv effect on the tri mesh at the interface. For elements with quality under 0.3 or 0.4 you can use the normal smoother as it aims for individual quality.

4) Open hexa mesh and hit merge. Btw. a geometry is not required for the further proceeding.

5) Merge hexa and tet under merge nodes ->Merge volume meshes. The surface mesh at the interface has to be in the same part e.g. "interface". Select it and apply.

6) Check mesh to identify any errors. Multiple edges should be reported at the interface.

7) Delete shell elements of the interface. Check again. This should give you no error when both volume meshes where in the same part e.g. fluid.

8) Smooth volume mesh again for better quality near the interface.

I have successfully applied this method many times over the last few weeks myself. It actually worked every single time;). The only problem that occured were some wrong associated shell elements near the interface. These can be easily assigned manually to the right part.

 Sixkillers October 30, 2013 04:52

Also take a look at tutorial called "Merged Tetra-Hexa Mesh in a Hybrid Tube" in ANSYS ICEM CFD Tutorial Manual. You might find it useful.

 AA29 January 21, 2015 19:15

Hi guys,

I have a hex and tet mesh and want to merge these two meshes to make one volume mesh(or region) WITHOUT the shell elements at the interface.
I am trying to follow the steps mentioned by kad, but still once I merge the volume mesh, I works ok without errors. I can see pyramids as they should be at the interface, but the shell elements are still there. If i delete the shell elements and do checkmesh i get the error of missing internal faces.

Am i missing something here?

Thanks